Inventor Help Constraining to Construction Line

[slegger]

Hi,

This is a hard one to explain so I will give and example:

normally if i have to do a bolt pattern and the hole has to be off center (e.g 45 deg) I would draw a vertical construction line then another costruction at 45 deg then General Dimension to constrain it. Then i would place a Point on the 45 deg construction line with a Aligned Dim for the P.C.D and it would be fully constraint. But now i cannot get the point to constrain to the construction line, is there a setting for this or a hotfix that i need?

I am runng Inventor Professional 2009 32-bit on Windows XP SP 2.

I hope this make sense basicly i just need to know how to constrain a point to a construction line.

Thank You

[shift1313]

Welcome aboard. Few questions for you on this. Im trying to think of an instance when you would need to start with a hole rotated 45 degrees but cant think of any(that doesnt mean anything, just im not thinking ).

 

A few things you can do to start with. If this is your first sketch or your part has been planned around the origin. You can project the X, Y or Z axis into your sketch as an angular reference.

 

I just tried this with a few different methods with no issues. One thing you dont need to do is add any points. You can add constraints to end points.

 

So just a quick step by step.

 

Start a sketch.

 

Project the Y axis into your sketch(this varies depending on what your sketch plane is).

 

Draw your line at roughly the right length/angle.

 

Dimension it(click Dimension, click the line and then hover the mouse around until the ordinate icon shows up and you can dimension the length of this line), add the angle.

 

Draw a circle( the center point will be yellow except when it "snaps" to something. if you start the circle at the endpoint of the line it will be constrained to it.)

 

Dimension the circle.

 

Im not sure what your cad experience is so if you wanted more or less info let me know:) that answer was pretty general

[slegger]

Thanks shift1313,

Thanks for the tip on projecting axis on sketck plane never thought of using that one and i have only been working with inventor for 4 years. I am also having trouble with drawing lines from projected center point, it will not give me a automatic vertical or horizontial from drawing off center point (eg line turn black drawing of Center Point). This has worked fine for many years but now is playing up and annoying when you have to manually add vert/horz constraint. I think the both problems are related and may be just a setting but can not find.

i attached a file showing what im trying to do - normally the point would snap on and constrain itself to the construction line.

part 1.zip

[shift1313]

well in the file you sent, i would get rid of the point on your 45degree line since its not needed and dimension your line to 18 instead. Also dimension your vertical reference line. Once you cut the hole through your part, do a circular array of the feature(not the sketch). This will be a better way to model and update this.

 

As far as your settings go. Up on the ribbon where your constraint buttons are there are two buttons. They are constraint inference and persistance. This can also be controlled with the CTRL button while sketching. To change which constraints these apply to, in a sketch with nothing selected, right click. The menu should have a Constraint Options listed. That will pop up the window you see in the image below.

 

If this flange is somewhat consistent but you change size you can create an easily modifiable part for the future. Are these each 1-offs or something standard. Also if these are pipe flanges, there are some in content center

[slegger]

Thanks Shift1313 the constraint thing worked perfect. Back to normal. As for the flanges unfortunately inventor doesn’t have a lot of Australian Standards in the library. i dont have a ribbon is that new to inventor 2010? i tried it on autocad did like it much.

again thankyou for you help

[shift1313]

Honestly I cant remember. I thought I had it in 2009. It was definitely in Acad 09. I really like it. I use Solidworks more than inventor and its user interface is similar. Once you get used to it, it can be very efficient.